What's new
What's new

Haas production lathe, CAM pairing

mikesparts

Plastic
Joined
Jan 27, 2017
Hey guys first post but have been creeping around, soaking in the knowledge for a while. I am an engineer at a very small manufacturing center and our machining group runs three HAAS turning centers (DS 30's). We geared up for high throughput and automation when purchasing the equipment so they all have bar feeders, parts catcher, Fanuc interfacing, rotary accumulators etc. We're about 6 months into production and things are starting to pick up in all areas of our facility except for machining. We're struggling to hit 60% uptime on the turning centers and most of this is due to changing over between runs. We got pretty good at making a few different widgets over the last few months but now as we try to introduce new widgets with even the slightest variation of the ones we already make it is stopping us dead in our tracks. Our business seems to be going in the direction of lower volume higher margin items so this downtime is becoming more common and it's killing us. Also a note, we make VERY basic turned parts, 75% of our machining is center drilling 2" round 1018, milling a flat across it and parting it off.

We've been using Autocad LT and manually programming the machines to get us going, knowing that we would eventually be upgrading and with all this downtime it looks like that time us upon us. We've been meeting with vendors and are leaning toward Solidworks and looking for a CAM software to pair with it. Does anyone have any experience or recommendations for a software that is geared toward high production and can incorporate these auxiliary processes like barfeed, handoff, parts catch etc? Nobody seems to be able to tell us with any confidence that the product they are repping can do these things.
 
Hey guys first post but have been creeping around, soaking in the knowledge for a while. I am an engineer at a very small manufacturing center and our machining group runs three HAAS turning centers (DS 30's). We geared up for high throughput and automation when purchasing the equipment so they all have bar feeders, parts catcher, Fanuc interfacing, rotary accumulators etc. We're about 6 months into production and things are starting to pick up in all areas of our facility except for machining. We're struggling to hit 60% uptime on the turning centers and most of this is due to changing over between runs. We got pretty good at making a few different widgets over the last few months but now as we try to introduce new widgets with even the slightest variation of the ones we already make it is stopping us dead in our tracks. Our business seems to be going in the direction of lower volume higher margin items so this downtime is becoming more common and it's killing us. Also a note, we make VERY basic turned parts, 75% of our machining is center drilling 2" round 1018, milling a flat across it and parting it off.

We've been using Autocad LT and manually programming the machines to get us going, knowing that we would eventually be upgrading and with all this downtime it looks like that time us upon us. We've been meeting with vendors and are leaning toward Solidworks and looking for a CAM software to pair with it. Does anyone have any experience or recommendations for a software that is geared toward high production and can incorporate these auxiliary processes like barfeed, handoff, parts catch etc? Nobody seems to be able to tell us with any confidence that the product they are repping can do these things.

Any top end CAM system will be able to handle bar feeds, hand offs etc. It's really not all that complex. Who have you been talking with? Seems odd that someone in the CAM industry that does lathe would not have those functions.
If you want to talk automation, look at Esprit. It will be standalone CAM so I would have this in addition to SW. If you're on a budget look at adding HSMWorks to SW or standalone Fusion360....(although I'm not sure how well F360 does lathe)
 
Fusion 360 doesn't do lathe worth shit, it's loosely functional in Inventor HSM as it is. good enough for now but in need of improvement.

I'm hesitant to add anymore CAM software in the future, but if we get advanced turning center (M/Y live tooling axes) then I might.

I would recommend comparing the features of Edgecam Turning, and ESPRIT SolidTurn, these are two high end dedicated CAM with complete feature sets.

That being said, I'm not sure this will solve your low volume, high variety issues... what you need for that is a TOOLING approach as well. Capto all the turning stations, measure every tool and get them within a few thou in all positions, and use macros/subroutines to load in tool offsets automatically for each changeover. doing this you can get your setup time under 20 minutes, even in precision small parts with 5 tools, under 30 minutes for 7 tools, etc.

combine a fast setup procedure with a fast CAM solution and you should be off to the races.
 
Thanks guys, I'm looking into those recommendations now. We've met with a guy from CAMWorks and it was pretty impressive, during our demo we sent him our most complicated part and within a couple minutes he had the program posted, minus the automation aspects. He wasn't sure how to add them, or if it was possible and it made us start to question if it was the right direction to go. We have also talked to someone from Mastercam but not in depth yet.

I should have been more descriptive when I said a variety of parts, we run highly similar parts and have them segregated by machine. For example, our first machine will turn 2" round 1018, center drill a 1.25" Dia hole then part it at 2" length. The next piece we run on it could be 1.75" round 1018 with a 1.00" dia center drill and then parted at 1.5" length. This is a "drastic" changeover for us and would probably take us out of commission for a day and if we wanted to go back to the first part we would lose another day, it is like we start all over from scratch again.

I've been working to standardize our turret setups and the types of pieces we run on each machine, so that changeovers from piece to piece may require at the most a radial drill end mill be changed to a drill bit or something similar but no real tooling moves. This has helped a bit but I still feel like we've got massive room for improvement, especially when bringing in new parts. In the situation from before, 2" round 1018 1.25" bore and 2" part length, our next part to make was exactly the same but 1" long instead of 2". That change took us out of production for 7 hours and then ran for less than an hour, as it was a short run we needed to do. We don't want to make 20 different pieces from each machine every day but we think 2-3 very similar parts should be able to be run in one day.
 
belay my previous recommendations, you need to hire a better machinist first.

maybe even think about ditching a CNC and drop a couple manual lathes in there. hilariously enough, for that kind of work they could be much faster.
 
belay my previous recommendations, you need to hire a better machinist first.

maybe even think about ditching a CNC and drop a couple manual lathes in there. hilariously enough, for that kind of work they could be much faster.
X2 on finding a better machinist, it should not take 7 hours to change a part length from 2" to 1"... That's, at most, a 5 minute change, even modifying the program longhand.

Josh

Sent from my XT1093 using Tapatalk
 
Things sound very fishy. What you want to do is simple. I would have someone come in and teach you guys the correct way to do things. Here we can change all 12 tools in a turret re-program a complex part by hand. Change and bore new jaws in about 3-4 hours top.
 
Athack, this is why it's starting to get scrutinized pretty heavily, things aren't adding up. Our head machinist is an old school guy who would gladly tell you he can run the hell out of a manual lathe but wont admit he's struggling to program these more automated machines. I think he could probably program it to run one part just fine but to add in the bar feeds, handoffs, backside turning etc, is more than we're capable of doing. This is why we want to be sure the turning software that can incorporates this stuff.
 
I have an idea of what could be happening here. You said you have a DS30 Haas and it's taking 7 hours to change a job...sound like you are doing an unnecessary pickup op. The wasted time is your guy fucking around with the sub spindle pickup op. A lot of places get caught up in the 'I have this tool so I must use it' approach. Small runs are often easier to run as op1, op2. Yes, CAM can generate all the code you need to do these pickup ops but you still need to know how to program them. If you're guy is having issues now just wait till you throw CAM at him. Sounds to me like you need to bring a consultant in at this point then have employees learn after the machines are making money.
 
I would agree, stay away from the autodesk turning products that come from the hsmworks core. The Delcam side of autodesk may be very good such as featureCAM. The HSMWorks products don't handle turning very well and there is no sign of that changing. You will also be likely to find very little support for it if you did get it also. It sounds like you will need support every bit as good as the software to get you up to speed.
 
For the type of work that you describe, you need to read up on using macros. It will be easier and faster that cam software.
 
Let's see, if the work you're describing is accurate:

-Centre drill doesn't change
-Drill depth changes so one Z depth and a tool comment
-Part-off length changes so another Z depth changes
-Run an endmill along a Y to cut a flat with Z depth changes

In total three values are changed and these change overs are taking you all day?

Save the money you'd spend on a CAM system and get an experienced lathe guy in to train you how to run what you've got. You could try standardizing your jaw depths so a single bit of copy pasted code to any of the programs would execute a safe sub hand off but it sounds like you'd be better off just breaking it into two ops at the rate you're currently going.
 
Thanks guys, I think the most time consuming item for them is getting the bar feeder setup correctly from piece to piece. We only do a sub spindle hand off on about 25% of our parts, though it should be more.

We do have Macros on the machines but I'm sure we aren't using them to their potential if we're using them at all. From what I've read on them and it seems like they would allow you to run one program for a family of simpler parts and change from an old piece to a new one by updating a couple variables? Before we started down this CAM road I was thinking of putting together a spreadsheet where we could just plug in any changes to dimensions and it would spit out the new numbers to put in the program but I think the macros could take the place of that if I'm understanding it correctly.
 
Besides using macros, I've had good luck customizing Haas's Visual Quick Code to spit out programs that are largely the same, with minor changes (variations in a part family, etc). May want to check that out.

M
 
Yes, a good macro program will have variables for each dimension change. Then use sub program calls for the sub spindle hand off and bar feed. The sub programs should be set up with variables noted in the program. Then the operator can make the required changes on the machine in a matter of minutes.
Like others have said, save your programs so that when your repeat work is back you just reload the program. Use notes in the header for the operator such as sub position bar feed position, ect..
 
Some more detail on my VQC setup:

First ops had two general templates in VQC for each part style, one for std (with option for extended nose) and one for secondary-drilled parts (also with option for extended nose). Had a barfeeder and parts catcher for first op, ran soft jaws with serrated pads to grip the bar stock.

Second op had a template for OD rough, c'drill, drill, OD turn, for each style in each part family (was making Swiss-style collets/bushings). Then inserted another template (if needed) at the end to finish the bore. Had templates for each type of collet/bushing (by size), as well as each style of part (std/extended nose). Got to be so I could change over from one part to the next in very short order, often just by changing a drill and touching it off, and spitting out a new program based on the VQC template.

The templates had some basic math for spindle speeds, based on drill diameter and a standard SFM value; as well as changing coordinate offsets based on a known starting point and the overall length of the part (calculated based on base + any extension).
 
Thanks guys, I'm looking into those recommendations now. We've met with a guy from CAMWorks and it was pretty impressive, during our demo we sent him our most complicated part and within a couple minutes he had the program posted, minus the automation aspects. He wasn't sure how to add them, or if it was possible and it made us start to question if it was the right direction to go.

A lot of folks here don't seem to like Camworks, but I've been using it for 10 years and it does lathe and mill/turn pretty good as far as I'm concerned. To do what you call "automation" (bar feeds, spindle swapping, or any other non-cutting code) can be accomplished by customizing your post processor. They have functions you can create called "post-operations", which is only limited by your imagination. If they can do it for you, all the better. Otherwise you'll have to learn how to use the post generator, which takes a while.
 
Honestly you've gotten all the advice you need for the products you describe. Now it's just a matter of getting the right people to effect the changes.

Question is, are you that guy? Do you wanna be the hero and stick your neck out but learn to make the variable/macro driven part family programs you obviously need.... or do you wanna find a CAM package that will only help a bit?

New CAM package will help if the shop expands their horizons, if that's not the forecast then somebody needs to step up.

Sent from my SM-G920V using Tapatalk
 
All this talk of macros..:skep:

They have their place and are super useful and efficient but lets not forget you still have to generate the gcode by hand. What happens if the next part is unique? Hand coding is the best way to lose money...not only in the amount of time wasted creating the code but in the mistakes made and resulting bad parts or machine crashes. You wanna do macros, create the needed code in CAM and then 'marco-fy it, win win!
 








 
Back
Top